DPF model#

The DPF model provides the starting point for opening a result file. From the Model object, you can connect various operators and display results and data.

To create an instance of the Model object, import the pydpf-core package and load a result file. The path that you provide must be an absolute path or a path relative to the DPF server.

from ansys.dpf import core as dpf
from ansys.dpf.core import examples

path = examples.find_simple_bar()
model = dpf.Model(path)

To understand what is available in the result file, you can print the model (or any other instance):

print(model)

DPF Model
------------------------------
Static analysis
Unit system: Metric (m, kg, N, s, V, A)
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  structural_temperature: ElementalNodal Temperature
------------------------------
DPF  Meshed Region:
  3751 nodes
  3000 elements
  Unit: m
  With solid (3D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 1
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1

For a comprehensive model example, see Basic DPF-Core usage.

For a description of the Model object, see Model.

Model metadata#

To access all information about an analysis, you can use model metadata:

Type of analysis
Time or frequency descriptions
Mesh
Available results

This example shows how you get the analysis type:

model.metadata.result_info.analysis_type

'static'

This example shows how you get mesh information:

model.metadata.meshed_region.nodes.n_nodes
model.metadata.meshed_region.elements.n_elements
print(model.metadata.meshed_region.elements.element_by_id(1))

3751
3000
DPF Element 1
    Index:         1400
    Nodes:            8
    Type:       element_types.Hex8
    Shape:        Solid

This example shows how you get time sets:

time_freq_support =  model.metadata.time_freq_support
print(time_freq_support.time_frequencies.data)

[1.]

For a description of the Metadata object, see Model.

Model results#

The model contains the results attribute, which you can use to create operators to access certain results.

This example shows how you view available results:

print(model.results)

Static analysis
Unit system: Metric (m, kg, N, s, V, A)
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  structural_temperature: ElementalNodal Temperature

Model.results

Available results of the model.

Organizes the results from DPF into accessible methods. All the available results are dynamically created depending on the model’s class:ansys.dpf.core.result_info.

Returns:: results – Available results of the model if possible, else returns common results.
Return type:: Results, CommonResults

all types of results

Result provider helper wrapping all types of provider available for a given result file.

Examples

>>> from ansys.dpf import core as dpf
>>> from ansys.dpf.core import examples
>>> model = dpf.Model(examples.find_electric_therm())
>>> v = model.results.electric_potential
>>> dissip = model.results.thermal_dissipation_energy

Type:: Result

Examples

Extract the result object from a model.

>>> from ansys.dpf import core as dpf
>>> from ansys.dpf.core import examples
>>> model = dpf.Model(examples.find_simple_bar())
>>> results = model.results # printable object

Access the displacement at all times.

>>> from ansys.dpf.core import Model
>>> from ansys.dpf.core import examples
>>> transient = examples.download_transient_result()
>>> model = Model(transient)
>>> displacements = model.results.displacement.on_all_time_freqs.eval()

With the results attribute, choosing the time, frequencies, or spatial subset on which to get a given result is straightforward.

This example shows how you get displacement results on all time frequencies on the mesh scoping:

disp_result = model.results.displacement
disp_at_all_times_on_node_1 =  disp_result.on_all_time_freqs.on_mesh_scoping([1])

For an example using the Result object, see Choose a time scoping for a transient analysis.

For a description of the Model object, see Results.

API reference#

For more information, see Model or Results.